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# How to model Earphone in SolidWorks?

By Sudhir Gill on 16 Feb 15:49 17 answers 2389 views 13 comments

This is a tutorial for the model tutorial competiton and its about the Earphone model I have designed using surfacing methods. The model is here Earphone.

• over 1 year ago

This tutorial illustrates how to model an earphone using surfacing methods. Since a lot of persons doesn't know about surfacing model therefore i tried to perform every function step by step. If you have any problem struggling with that even after my efforts, just let me know. I will help you as much as I can.

1. ### Step 1

Start Solidworks in Part mode. Select front plane and then sketch.

2. ### Step 2

Draw entity using splines like this one. For this sketch i have used two spline and a centre line along right plane. The two splines are having tangent relation.

3. ### Step 3

Now select revolve surface under surfaces tab. Revolve the profile along the centre line.

4. ### Step 4

Under surfaces tab select Reference geometry >> plane. Now select Right plane as the first reference and offset it by considerable distance.

5. ### Step 5

Now select plane1 and then sketch.

6. ### Step 6

Draw a circle like this one.

7. ### Step 7

Under sufaces tab click Extruded surface.

8. ### Step 8

Extrude it in both direction with a considerable distance.

9. ### Step 9

Now select front plane and then sketch.

10. ### Step 10

Draw two spline cutting the surfaces.

11. ### Step 11

Under surfaces tab select trim surfaces.

12. ### Step 12

Select the surfaces under the splines and remove them.

13. ### Step 13

Under surfaces tab select lofted surface.

14. ### Step 14

Select both edges.

15. ### Step 15

Under Start/End constraints change start and end constraint to tangency to face. Click OK.

16. ### Step 16

We have basic shape of the earphone. I have decreased the radius of the extruded surface Because it was a little larger.

17. ### Step 17

Select section view in standard views.

18. ### Step 18

Select front plane for section and click OK.

19. ### Step 19

Under surfaces tab select offset surface.

20. ### Step 20

Select the top face and change the distance to minimum i.e. about 1.5mm in my case.

21. ### Step 21

Now select Top plane and then sketch.

22. ### Step 22

Draw a circle.

23. ### Step 23

Under surfaces tab select trim surfaces.

24. ### Step 24

Trim the inner portion of the top-most face.

25. ### Step 25

Again top plane and then sketch.

26. ### Step 26

This time draw a circle considerably smaller than last one.

27. ### Step 27

Select trim surface under surfaces tab.

28. ### Step 28

Select the outer portion of the offsetted surface.

29. ### Step 29

Click OK and the area is trimmed.

30. ### Step 30

Under surfaces tab select boundary surface.

31. ### Step 31

Select both edges.

32. ### Step 32

Select tangency to face for both edges.

Click OK.

34. ### Step 34

Now under surfaces or feature tab select reference geometry and then axis.

35. ### Step 35

Select top plane and origin. This will create an axis perpendicular to top plane and passing through origin.

36. ### Step 36

Now select top plane and then sketch.

37. ### Step 37

Make a circle for hole.

38. ### Step 38

Now click linear sketch pattern in sketch tab.

39. ### Step 39

Select the circle to entity to pattern.

40. ### Step 40

Adjust the distance and increase the number of instances.

41. ### Step 41

Now select circular sketch pattern.

42. ### Step 42

Now select the 2nd circle to pattern.

43. ### Step 43

Repeat the same step for other circles increasing the number of instances each time.

44. ### Step 44

Under surface tab select trim surface.

45. ### Step 45

Now select keep selection.

46. ### Step 46

Select the excluded surface of holes.

47. ### Step 47

Click OK and the surface is trimmed.

48. ### Step 48

Now select top plane and then sketch.

49. ### Step 49

Use slot tool to make 2 slots.

50. ### Step 50

Now select trim surface in surface tab and select remove selection. Select the surface bounded in slots and click OK.

51. ### Step 51

Now we have the space for the air.

52. ### Step 52

Select knit surface under surface tab.

53. ### Step 53

Select all surfaces one by one and then click OK.

54. ### Step 54

Under surface tab select thicken.

55. ### Step 55

Select the surface. It will select Knit surface feature. Change the thicken distance to 1mm and outside direction. Click OK.

56. ### Step 56

Now we have solid body of the earphone. We will now seperate the bodies.

57. ### Step 57

Select top plane and then sketch.

58. ### Step 58

Change view to hidden with shaded line.

59. ### Step 59

Offset the edge by 0.50mm and then draw two straight line horizontally. Trim other entities.

60. ### Step 60

Select revolved surface in surface tab.

61. ### Step 61

Select axis1 and click OK.

62. ### Step 62

Go to insert menu then feautres >> split.

63. ### Step 63

Select the revolved surface as the trim tool and click cut part.

64. ### Step 64

Now check both the bodies and click OK. This feature will generate two split bodies by the revolved surface.

65. ### Step 65

Now hide the revolved surface.

66. ### Step 66

Again select section view about front plane in standard view toolbar.

67. ### Step 67

Select reference geometry and then plane under surface or features tab.

68. ### Step 68

Select top plane and then offset it by a distance so that it will lie in the upper body.

69. ### Step 69

Select the plane2 and then sketch.

70. ### Step 70

Draw a circle larger than the region bounded by the holes.

71. ### Step 71

Under features tab click extruded boss/base feature.

72. ### Step 72

Under direction1 select up to body.

73. ### Step 73

Select the upper body and enable thin feature by a distance of 0.50mm. Click OK.

74. ### Step 74

Now we have the body for the speaker of ear phone.

75. ### Step 75

Now click file save.

76. ### Step 76

Enter any file name for the part document. I entered earphone for myself.

77. ### Step 77

After saving part click insert>>feature and then split.

78. ### Step 78

Again select revolved surface2 from the surface bodies under tree view and click cut part.

79. ### Step 79

Double click the cut body1 and save it.

80. ### Step 80

Repeat the same step for the other body and click OK.

81. ### Step 81

Now right click the split2 feature and then select create assembly.

82. ### Step 82

Click browse.

83. ### Step 83

Now save the assembly file for the splitted part document.

84. ### Step 84

Now the assembly file will open.

85. ### Step 85

Right click the upper body and select float.

86. ### Step 86

Move it and then rotate it to have a better view.

87. ### Step 87

Here is the rendered image of the earphone. This one is not much better than the last one but you can make one better if done with care.

• over 1 year ago

Please Click "it worked" friends :)

• over 1 year ago

Thanx Aykut Dana, Abhijeet & Krishna.

• over 1 year ago

Very good and very well detailed and documented one of the best I have seen yet on GrabCAD
//Handshake for work and effort
:)))))

• over 1 year ago

Great! Very detailed explanation, Thanks :))

• 6 months ago

Very Nice! Winning!!